[CfdUser5855]

Hi all,

I'm running a pimpleFoam case, and the error

'--> FOAM FATAL ERROR:
Attempt to cast type zeroGradient to type nutWallFunction

From function To& Foam::refCast(From&) [with To = const Foam::nutWallFunctionFvPatchScalarField; From = const Foam::fvPatchField<double>]
in file /home/ubuntu/OpenFOAM/OpenFOAM-7/src/OpenFOAM/lnInclude/typeInfo.H at line 114'

appears after initially solving for ux, uy, and uz. I have tried a number of different types for the patch to see if it will run, but the error appears each time with the different type used substituted into it.

A search for this error provides a link to people saying they have this problem, but no solution is working for me

My nut case is shown below

dimensions [0 2 -1 0 0 0 0];

internalField uniform 0;

boundaryField
{
#include "include/ABLConditions"

inlet
{
type zeroGradient;
//value uniform 0.0;
}

outlet
{
type zeroGradient;
//value uniform 0;
}

top
{
type zeroGradient;
//value uniform 0;
}

NiliDuneField
{
type nutkAtmRoughWallFunction;
z0 0.03;
value uniform 0;
}
}

If anyone is able to help with this, that would be greatly appreciated

[HPE]

The reason of that error is bad class hierarchy change. Spilled from OpenFOAM.org...

Please just use a nut wall function in 0/nut file.

For example, if you have `fixedValue` for a patch inside 0/nut, please change it to `nutLowReWallFunction`. Then it should run.

[CfdUser5855]

Thanks for the advice, however the error then throws up that the patch type for inlet must be wall, which isn't correct for this simulation

Do you know which nut type would resolve that issue, without changing the wall type?

[HPE]

would you mind to share the boundary condition files as well as constant/polyMesh/boundar*, please?

[CfdUser5855]

Sorry for being late getting back to you. I tried remaking the case to see if it was a redundant line that was causing the issue but no joy

My constant/polymesh/boundary is as follows

4
(
outlet
{
type patch;
nFaces 33775;
startFace 29542772;
}
inlet
{
type patch;
nFaces 28497;
startFace 29576547;
}
top
{
type patch;
nFaces 450;
startFace 29605044;
}
DuneField
{
type wall;
inGroups List<word> 1(wall);
nFaces 459920;
startFace 29605494;
}
)

p is as follows:

#include "include/initialConditions"

dimensions [0 2 -2 0 0 0 0];

internalField uniform $pressure;

boundaryField
{
inlet
{
type zeroGradient;
}

outlet
{
type uniformFixedValue;
uniformValue constant $pressure;
}

top
{
type zeroGradient;
}

DuneField
{
type zeroGradient;
}

ground
{
type zeroGradient;
}


u is as follows

#include "include/initialConditions"

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type atmBoundaryLayerInletVelocity;
#include "include/ABLConditions"
}

outlet
{
type inletOutlet;
inletValue uniform (0 0 0);
value $internalField;
}

top
{
type zeroGradient;

}

DuneField
{
type uniformFixedValue;
value uniform (0 0 0);
uniformValue constant (0 0 0);
}

k is as follows

#include "include/initialConditions"

dimensions [0 2 -2 0 0 0 0];

internalField uniform $turbulentKE;

boundaryField
{
outlet
{
type inletOutlet;
inletValue uniform $turbulentKE;
value $internalField;
}

inlet
{
type atmBoundaryLayerInletK;
#include "include/ABLConditions"
}

top
{
type kqRWallFunction;
value uniform 0.375;
}
DuneField
{
type zeroGradient;
}
}

nut is as follows

dimensions [0 2 -1 0 0 0 0];

internalField uniform 0;

boundaryField
{
#include "include/ABLConditions"

inlet
{
type nutLowReWallFunction;
value uniform 0.0;
}

outlet
{
type nutLowReWallFunction;
value uniform 0;
}

top
{
type nutLowReWallFunction;
value uniform 0;
}

DuneField
{
type nutkAtmRoughWallFunction;
z0 0.03;
value uniform 0;
}
}

epsilon is as follows

dimensions [0 2 -3 0 0 0 0];

#include "include/initialConditions"

internalField uniform $turbulentEpsilon;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0.01;
}
outlet
{
type inletOutlet;
inletValue uniform $turbulentEpsilon;
value $internalField;
}
top
{
type epsilonWallFunction;
value uniform 0.01;
}
DuneField
{
type zeroGradient;
}
}


Thank you very much for looking at this

[HosamAlrefaie]

Hi CfdUser5855,

have you solved this?

[sunafegon]

Hi everyone,

I've encountered this issue as well. Has anyone found a solution?

Much appreciated.

[Bloerb]

Check your polyMesh boundary file. Make sure that walls are of type wall and not patch.

[sunafegon]

Originally Posted by Bloerb

Check your polyMesh boundary file. Make sure that walls are of type wall and not patch.

Hi Bloerb, I think that aspect of the issue has already been solved. It's now turned to the issue of it demanding that the inlet and outlet patches be of type wall instead of type patch, which isn't correct for the study type. I'm not sure if it makes a difference to the calculation, however. Maybe it doesn't matter if the inlet or outlet are type patch or type wall given the equations used to define the conditions. Any thoughts?

Thanks.

[vonboett]

I had the same problem... so here is the simple solution:


just still use:

type calculated; value uniform 0.0


for a patch and wallFunctions for walls.

[esma]

In my case, the issue was the patch type in one of the boundaries wasn't corrected between wall to patch or vice-versa in epsilon setup. The solver gives an error on "nut" doesn't mean the error is in nut could be in omega/epsilon depending on your turbulent model.